[AlmostSurelyRob]

I am playing with the new twoPhaseEulerFoam. We developed a general population balance class as a diameterModel similar to IATE model but we plan to have different methods there. For now we have some good comparisons with analytical solutions for the method of classes but would like to go to method of moments of various forms.

We are really trying hard to follow minimalilty of code and future maintainability, so we believe we have a fairly well abstracted class structure. The twoPhaseEulerFoam solve is untouched and we only add our PBE library to controlDict in order to make our PBE diameter model selectable.

So far so good.

I really like the current implementation of twoPhaseEulerFoam but I still haven't grasped everything. In particular I still haven't dived into thermophysical side of it which is fairly new to me. Thermophysics shouldn't be really playing any role in my PBE cases so I am trying to suppress it as occasionally my cases diverge because of energy equation. Is there a way to do it?

At the moment I switched off all interfacial terms related to temperature and fixed temperature or each boundary of my domain to constant uniform value. Same for internal mesh.

My `thermophysicalProperties' for both phases

thermoType
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleInternalEnergy;
}

as I want both of my phases to be imcompressible for testing purposes. This still causes small fluctuations of temperature and an occasional 1000 iterations in the water phase energy equation. On some runs this leads to a simulation crash.

At the moment I just set under relaxtion to 0 and will see how this works, but is there a way to actually supress completely the solution of the energy equation under the new solver without changing the code of the solver?

[bsoubelet]

Hello,

Due to repeating crashes with twoPhaseEulerFoam and the energy equations also, we found a way around by by-passing the solution of these equations in the fvSolution file:

    "e.*"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        //tolerance       1e-7;
        relTol          2;
        minIter         0;
    }

This way you don't solve at all the energy equations, but you don't have to re-write the code.
After several thousands of iterations, I was able to switch them on again with:

    "e.*"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-7;
        relTol          0;
        minIter         1;
    }

Hope it will help!

[sharonyue]

Originally Posted by bsoubelet

Hello,

Due to repeating crashes with twoPhaseEulerFoam and the energy equations also, we found a way around by by-passing the solution of these equations in the fvSolution file:

    "e.*"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        //tolerance       1e-7;
        relTol          2;
        minIter         0;
    }

This way you don't solve at all the energy equations, but you don't have to re-write the code.
After several thousands of iterations, I was able to switch them on again with:

    "e.*"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-7;
        relTol          0;
        minIter         1;
    }

Hope it will help!

Um, thats quite smart. haha. Interesting.

[aee]

Robert,
Could you elaborate a bit on your PBE implementation?

I would like to model emulsion separation in the presence of surfactants, and am feeling pushed towards a PBE solution rather than a modification of the IATE model.

Would you be willing to share code?

Andrew

[BlnPhoenix]

I used this work around succesfuly in OF2.3.x. Now that i wanted to do the same in OF3.0.1 it doesn' t work anymore.

When i set:

"e.*"
{
solver smoothSolver;
smoother symGaussSeidel; //
tolerance 1e-7;
relTol 2;
minIter 0;
}

The solver is still solving for "e.air" and "e.water" and calculating "min T.air" and "min T.water". Normally that would not bother me but i suspect it to be the reason twophaseeulerfoam crashes after 4.3 seconds of simulation time.

Is there another possibilty to turn off energy in twophaseeulerfoam OF3.0.1?

[ali.m.1]

You can use reactingTwoPhaseEulerFoam, and make the problem isothermal.

This is done by using 'pureIsothermalPhaseModel' in constant/phaseProperties.

[BlnPhoenix]

Thanks. I will look into that.

I also found out that setting air phase diameter model to "constant" and setting min inter for e.water and e.air to "0" yields quasi-isothermal running. Temperatures are constant during solving.

[rdbisme]

Originally Posted by BlnPhoenix

I used this work around succesfuly in OF2.3.x. Now that i wanted to do the same in OF3.0.1 it doesn' t work anymore.

When i set:

"e.*"
{
solver smoothSolver;
smoother symGaussSeidel; //
tolerance 1e-7;
relTol 2;
minIter 0;
}

The solver is still solving for "e.air" and "e.water" and calculating "min T.air" and "min T.water". Normally that would not bother me but i suspect it to be the reason twophaseeulerfoam crashes after 4.3 seconds of simulation time.

Is there another possibilty to turn off energy in twophaseeulerfoam OF3.0.1?

I'm in the same situation. Did you figure it out how to shut down energy?

[BlnPhoenix]

Hi,

yes, i think i tried what i posted on January 11th:

Originally Posted by BlnPhoenix

Thanks. I will look into that.

I also found out that setting air phase diameter model to "constant" and setting min inter for e.water and e.air to "0" yields quasi-isothermal running. Temperatures are constant during solving.

You can try that also. And don't get confused that the solver will show actual temperatures. They should remain constant though during the simulation. Don't forget also to set the same temperature for each phase, e.g. 300 K.

[rdbisme]

Originally Posted by BlnPhoenix

Hi,

yes, i think i tried what i posted on January 11th:



You can try that also. And don't get confused that the solver will show actual temperatures. They should remain constant though during the simulation. Don't forget also to set the same temperature for each phase, e.g. 300 K.

Thanks for the answer!

Yes, I tried that but I still get

smoothSolver:  Solving for e.*, Initial residual = 0.997813, Final residual = 0.000848293, No Iterations 6

messages. It seems that the solver ignores the minIter 0 and still solves the energy equation.

The temperature fluctuates around the 300K.

[BlnPhoenix]

Hm, if u have set both diameter models to constant i'm afraid i don't know what's causing this. Maybe instead of "minIter" you can try "maxIter"?! Sorry that i can't be of any better help.

[rdbisme]

Originally Posted by BlnPhoenix

Hm, if u have set both diameter models to constant i'm afraid i don't know what's causing this. Maybe instead of "minIter" you can try "maxIter"?! Sorry that i can't be of any better help.

Thanks for your answer. I will check on that!

[rdbisme]

Originally Posted by ali.m.1

You can use reactingTwoPhaseEulerFoam, and make the problem isothermal.

This is done by using 'pureIsothermalPhaseModel' in constant/phaseProperties.

I also managed to avoid energy equation solving with following settings in fvSolutions:

"(h|e).*"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1;
        relTol          0;
        minIter         0;
    maxIter        0;
    }

It's somehow hacky but does the job.

[ali.m.1]

Hey

Has anyone managed to make the solver not solve alphat? I don't want temperature to be solved at all, but this still has values, which means it must be affected somehow?

Cheers

Ali

[rdbisme]

Originally Posted by ali.m.1

Hey

Has anyone managed to make the solver not solve alphat? I don't want temperature to be solved at all, but this still has values, which means it must be affected somehow?

Cheers

Ali

alphat is the turbulent thermal diffusivity. It's retrieved from the turbulence model. With the post just before yours you can make the solver to not solve the energy equation (so related to temperature).

What are you trying to achieve?

Sent from my LeTv x500 (BB72 ROM)

[ali.m.1]

Hi

Thanks for the information.

The temperatures do not change anymore with the above post, so thanks for that.

I'm trying to model a slurry flow (2 phase) submerged jet impingement, but the solver is struggling to converge. I'm just looking for tips for convergence!

It seems to be the turbulence which is blowing up all the time, as omega (KOmegaSST) is up to 1000ish.

Alasdair

[rdbisme]

Originally Posted by ali.m.1

Hi

Thanks for the information.

The temperatures do not change anymore with the above post, so thanks for that.

I'm trying to model a slurry flow (2 phase) submerged jet impingement, but the solver is struggling to converge. I'm just looking for tips for convergence!

It seems to be the turbulence which is blowing up all the time, as omega (KOmegaSST) is up to 1000ish.

Alasdair

As a general suggestion checklist:

1. Check your mesh (run checkMesh utility). Too high aspect ratios produce lots of troubles. Check also orthogonality.
2. Check BCs.
3. Try to use the adjustableRunTime constraint on the time-stepping with a low target Courant number (0.5 or lower)
4. try to use diffusive schemes (i.e. upwind)

Let us know how it goes and if you manage to solve the problem (and how!!)

[hooman.4028]

Originally Posted by tidusuper91

As a general suggestion checklist:

1. Check your mesh (run checkMesh utility). Too high aspect ratios produce lots of troubles. Check also orthogonality.
2. Check BCs.
3. Try to use the adjustableRunTime constraint on the time-stepping with a low target Courant number (0.5 or lower)
4. try to use diffusive schemes (i.e. upwind)

Let us know how it goes and if you manage to solve the problem (and how!!)

Hello Ruben,

I have problems using twoPhaseEulerFoam/reactingTwoPhaseEulerFoam. My p_rgh blows up and my temperatures go to very high numbers. This is confusing to me, since I set maxIter and minIter both to zero for h/e equations. Can you please guide me on this? Relaxation factor: 0.5, maxCo 0.5. OF 4.1.


Thanks!

[rdbisme]

Originally Posted by hooman.4028

Hello Ruben,

I have problems using twoPhaseEulerFoam/reactingTwoPhaseEulerFoam. My p_rgh blows up and my temperatures go to very high numbers. This is confusing to me, since I set maxIter and minIter both to zero for h/e equations. Can you please guide me on this? Relaxation factor: 0.5, maxCo 0.5. OF 4.1.

Thanks!

Dear hooman, generally that means that something wrong is happening. Describe better your geometry and the boundary conditions you configured on it.

Most probably the computation is diverging somewhere else influencing also the value of the temperature somehow.

Try also to post an excerpt of the log so we can see what is happening...

Sent by my Honor 8 using Tapatalk

[hooman.4028]

Originally Posted by tidusuper91

Dear hooman, generally that means that something wrong is happening. Describe better your geometry and the boundary conditions you configured on it.

Most probably the computation is diverging somewhere else influencing also the value of the temperature somehow.

Try also to post an excerpt of the log so we can see what is happening...

Sent by my Honor 8 using Tapatalk

I appreciate the quick response. It is a simple fluidized bed case (3D). The files are in the following link:

https://www.dropbox.com/s/2lrcoyzymx...files.rar?dl=0